Datasheet
14 CHAPTER 1 INVENTOR DESIGN PHILOSOPHY
Using DWG Files in Inventor
You can use DWG files in a number of ways in Inventor. Although Inventor does not support the
creation of AutoCAD entities, you can utilize AutoCAD geometry in Inventor sketches, Inventor
drawings, title blocks, and symbol creation.
When creating a new part file in Inventor, you can copy geometry directly from an AutoCAD
DWG and paste it into an Inventor sketch. AutoCAD dimensions will even be converted into fully
parametric Inventor dimensions. However, only minimal sketch constraints will be created when
doing this. Using the Auto Dimension tool within the Inventor sketch environment, you can apply
sketch constraints to the copied AutoCAD data quickly. It is important to remember that many
AutoCAD drawings contain fundamental issues such as exploded or ‘‘fudged’’ dimensions and
lines with endpoints that do not meet. Copying such drawings into an Inventor sketch will of
course bring all of those issues along and will typically provide poor results.
Another way to use AutoCAD data in Inventor is in an Inventor DWG file. Often you’ll have
symbols in AutoCAD in the form of blocks that you want to use on a drawing in Inventor, such as
a directional flow arrow or a standard note block. Although you could re-create these symbols in
Inventor, you can also simply copy the block from AutoCAD and paste it into the Inventor DWG.
This functionality exists only within an Inventor DWG and is not supported in an Inventor IDW.
In fact, it is one of the few differences between an Inventor DWG and an Inventor IDW.
Mechanical Desktop DWG files can be opened or linked into Inventor assemblies. When the
Mechanical Desktop file is opened in Inventor, options allow the translation of Mechanical Desk-
top models into parametric Inventor parts and assemblies, as well as fully associative layouts
into Inventor drawing files. When the Mechanical Desktop file is linked into an Inventor assem-
bly, it behaves similarly to an AutoCAD XRef, and all edits will be maintained using Mechanical
Desktop.
Creating DWG Files from Inventor Drawings
Users of Inventor may often find that they are called upon to create native DWG files from Inven-
tor IDW files for use by customers or other people within the company. A user may create a DWG
file by simply performing a Save Copy As and saving it as an AutoCAD DWG file. The newly
created DWG file will not be associative to the Inventor part or assembly or IDW file and will not
reflect any changes made to the part, assembly, or Inventor drawing file. It is common to use Save
Copy As on an Inventor drawing and save it to an AutoCAD DWG just before making revision
changes, thereby preserving a copy of the drawing in a static state at that revision level. Once
the static copy is saved, revision edits can begin, and the original Inventor drawing will update
automatically.
Beginning with Inventor 2008, users have the option of creating a native Inventor DWG file in
place of the IDW file. This DWG file will behave exactly like an Inventor drawing file, except that
the file extension will be .dwg instead of .idw. Just like an IDW file, an Inventor DWG file will
update whenever parts or assemblies linked to the file are changed and updated. Note too that if
you have IDW files that were created in a version of Inventor previous to Inventor 2008, you can
save those files as fully associative DWG files so that your drawing library contains one consistent
drawing file type. This process can even be batched and scheduled to run overnight using the
Task Scheduler, which you can open by selecting Start All Programs Autodesk Autodesk
Inventor 2010 Tools Task Scheduler.
You can open an Inventor DWG file in AutoCAD and edit it with some limitation. The primary
limitation is that the Inventor objects are protected from modification. AutoCAD dimensions and
other entities can be added and will remain intact when the file is opened again in Inventor, but
as a rule, objects must be edited in the application from which they were created.